Automatic Symbol Creation in Altium 365
We sincerely believe that this guide has inspired you to create your own project. However, in order to design your projects, you will need a set of components created that form the functionality of your future device. Earlier in this guide, you used the provided cloud library in which all the necessary components had already been added. Although the integration of Octopart with Altium Designer includes a large coverage of the component base, they cannot cover absolutely all the components in the world and there is a possibility that nobody has yet created the component that you require. Therefore, you need to be able to create components for the library manually. As already described in the first chapters of this guide, each component of the library consists of a symbol, a footprint, models, and a set of additional parameters. Within this section, we will completely create GSB343K33HR and MBT3904DW1T1G components, including their symbols and footprints. The GSB343K33HR component will be created in Altium 365 and will have all the benefits of this system, such as access from anywhere, the possibility of collaboration, and always up-to-date information from component suppliers. The MBT3904DW1T1G component will be created in the local library using the traditional approach. The component object creation tools, such as Symbol Wizard and IPC Compliant Footprint Wizard that are described later in the chapters of this guide are available for both approaches, but we highly recommend you use the approach using Altium 365. In this chapter, we will create a symbol for our component.
Let’s start creating GSB343K33HR in Altium 365.
Connect to the required workspace then select File > New > Component from the main menus. The Create new component dialog that opens allows you to specify the type of the component to create. We’re creating a USB 3.0 connector, so select Connectors in the list as a component type then click OK.
Tip: The list of component types is defined on the server and can be changed on the Data Management - Component Types page of the Preferences dialog.
The editor that opens is the starting point for Altium 365 component creation. This editor requires you to specify the name of the component, its description, parameters, symbol and footprint, datasheet, and possible part choices. First of all, let's specify the name, description, and set of parameters for our component. This can be set very quickly using the Manufacturer Part Search panel. Open the panel by clicking the ••• in the Name field to define the component name and parameters. In the Search field, enter GSB343K33HR, which is the part number of the required component then press Enter. Select the GSB343K33HR component from Amphenol Commercial then click OK.
Tip: If a selected component has the icon, there are already symbols and footprints created for it. They will be automatically imported to the component being created after clicking OK. If you wish to create them manually, just remove them. Also, these components can be placed directly into the project’s schematic or PCB using the Manufacturer Part Search panel.
The component symbol can be created either manually or by using the Symbol Wizard, which allows you to quickly create component symbols. In most cases, it is recommended to use the Symbol Wizard to create basic symbols for ICs or connectors. Manually creating symbols gives you more flexibility but it takes much more time and requires more attention. Creating symbols manually is described in Chapter 5.2. This component will be created using the Symbol Wizard. Click the Wizard button below the Add Symbol icon in the Models region to open the Symbol Wizard dialog and begin creating a new symbol.
The GSB343K33HR component is a 12-pin connector. For convenience, in the schematic design, all the pins of components of the "Connector" type are usually placed on one side and this component is not an exception. In the Symbol Wizard, in the Number of Pins field, enter 12 (or use the arrows to select). Use the Layout Style drop-down to select Single in-line. The grid in the Symbol Wizard is used to assign a Group, Display Name, Designator, Electrical Type, Description, and Side for each pin.
For each pin of this symbol, we need to specify the Display Name and Electrical Type parameters.
The Display Name is the actual pin name that will be shown inside of the symbol body near the corresponding pin. Usually, the pin name describes a specific function of the device for its proper connectivity on the schematic. Click on the field in this column for the desired pin and enter the name for it.
The Electrical Type is the I/O type of the pin, which will help to find possible connection errors during project validation. For example, an error will occur when two pins with Output type are connected to each other. The Electrical Type is selected by using the drop-down menu then select the required type. The preview that is displayed on the right side of the dialog shows the current symbol view.
Define the pin parameters as shown in the figure below. After adding and configuring all the pins, click OK to save the symbol and assign it to a created component.
Tip: Add an \ symbol after the letter of the pin name to add an upper line.
Note: Always pay a great amount of attention to the accurate and proper pin name definition! Your symbol should represent actual component pin functions and any errors will result in an incorrect connection to the component and disrupt functionality.
After clicking OK, a new tab opens in the main design space with the generated symbol displayed. This tab allows you to completely customize its appearance. Let's change the pin length and font to make this symbol visually correspond to other symbols in the library. Using right-to-left selection, select all pins. In the Properties panel, change the Pin Length value to 200 mil. Expand the Font Settings region of the panel then enable the Custom Settings boxes for Designator and Name to unlock editing for font settings. Using the Font Settings drop-down, define Arial as the font for both.
Tip: You can change measurement units by selecting Tools > Document Options from the main menus then choosing mm or mils in the Units region.
You may notice that there is a crosshair of black lines in the center of the symbol editor. Its purpose is to specify the point to which the symbol will be attached when placed from the Components panel. It is recommended to place the end of the first output of the component at this crosshair. Select the entire symbol and place it as shown in the figure below.
Save the symbol then close the symbol editor tab. The updated symbol now appears in the component editor. But the component is not complete yet since there is no footprint for it. A footprint for this component will be created in Chapter 5.3, so do not close this tab in order to access it in Chapter 5.3.
Tip: You can edit a symbol in the Component Editor at any time by pressing the icon in the upper-right corner of the editor. Also, the Symbol Wizard can be accessed by selecting Tools > Symbol Wizard when editing a symbol.